Re-use pattern
Re-use pattern let's us make use of pattern used in part to instantiate and assemble parts easily and quickly. Consider the plate shown below where one of the hole was created originally using hole command, while rest were simply patterned. Now, in an assembly, we are required to put bolts in all holes. To do this, we would only assemble one of the bolt in its place using constraints like offset, coincidence of the axis etc. And that is what is shown below, we assembled one bolt in one of the hole.
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| One bolt assembled with plate |
After that is done, we would use the tool i.e. Re-use pattern and assemble rest of the bolts in place by using the pattern. To create number of copies, you need to select Bolt as "Component to instantiate", under the "Pattern" section, you need to select any of the hole, this would enable to automatically pick up the number of instances and pattern information. The tool also displays a set of options like if you would like to keep link with pattern, whether components' position with respect to pattern's definition or generated constraints etc. You can see all these option below. Let's see what these options mean and how you can use this options.
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| Options available in Reuse pattern |
- Keep Link with the pattern - If you check this option, it will update the number of parts that you have used. For example, if number of pattern holes changed to five from six, the bolts would automatically reduce.
- Pattern's definition / generated constraints - If you use Pattern's definition, only the bolts and their positions will be copied using pattern information, but the constraints applied to the original instance will not be copied. If you use generated constraints, constraints of the original instance will also be automatically copied.
- First instance on pattern
- Re-use the original component - You will see that the original component is used and the total number of instances created are for the remaining positions only.
- Create a new instance - If you use Create a new instance, a new instance will also be created in the place where there's the original instance that you used for instantiation. So, there will be two copies in the place where there's the original instance.
- Cut and past the original component - This option will simply cut the original instance and paste it at all places. So, you will see name change and difference in the way pattern names.
For most of the time, you would be using Re-use the original component.
Save management: How to save files in Catia?
Normally, you may save files using Ctrl+S. While it's okay to use Ctrl+S when only part files are open, however if you are working with assemblies or if multiple part and assembly files are open, it's better to use save management. You can access save management using File > Save management.
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| Save management options |
Save management provides state of all file documents individually, so you can see which files have not been saved yet, which are saved, which are open etc.Any file which has not been saved, you would need to use the option save as for the first time and you can give a name of your preference. In an assembly, the files which are New, you can use Save as to save these files and give a name of your preference or, alternatively, you can use save / save as for the main assembly file, and all dependent documents i.e. parts or assemblies within that assembly will be automatically saved. So, when you use save for the assembly file, you need not use save as / save for the new files. In case the option Enable independent saves is selected, you would be able to save the main assembly file without saving the dependent part and assembly files within that assembly. So unless you want to save the dependent files individually, you should keep the option unselected.
How should you create revision files in Catia and avoid file conflicts?
Lets assume that you have an assembly with some parts in it, and you wish to create a revision assembly, that has some redesigned parts from this existing assembly. Now you may be tempted to copy the existing assembly folder and paste it with new name, and use these files for modifying parts and assemblies. However, this is not the right way to do it, for the reason that, all files in Catia have a UUID i.e. unique universal identifier. So when you copy a Catia file and save it in another location in windows (without opening Catia), the new file that you created will have same UUID as the files that you copied from (even if you rename the files). So you would not be able to use these files together in an assembly document without actually renaming it in Catia when it find conflicts in the UUID, because renaming it will then modify the UUID.
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| Part number conflict arising due to same UUID |
So the correct way to re-use file / assemblies in Catia i.e. to open assembly file in Catia and use Save management > Save as to save the copy of file in new location. If you have saved a new assembly file in new location, you can use the propagate directory option to save all associated dependent files in the new location automatically. This will create copies with new UUID.
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| New from applied on an assembly |
Alternatively, you can use File > New from to create copies of files, this will let you create a copy of the file and will change the UUID internally. This new file created can be saved without any conflicts. The dialogue box above show you all dependent file when you select it, so using arrow keys you can select if you wish to rename just the assembly file or also associated files with it.